How to paste a symbol onto a surface?

[who8myrice123]

Hi guys, I'm trying to paste a circular symbol onto an angled face/surface. The symbol came from a different part, so its position is way off. How would I move it directly onto the face I want?

Thanks for any help in advance!

 

[who8myrice123]

I also forgot to ask, how would I apply a text for engraving onto a curved surface?
I'm having difficulty keeping the text perfectly aligned with the surface.

 

[JohnRBaker]

If the 'symbol' can be found as character in a TrueType or OpenType font, then you can use the geometric 'Text' function to draw the symbol on the face of a model. BTW, what do you mean by "perfectly aligned with the surface"? Could you provide at least a pciture of what you're attempting to do?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[who8myrice123]

Thanks for the reply John! I actually figured it out.
I used Menu > Edit > Align > Best Fit or Point Set to Point Set to align the text and symbols with the part. And then I used Project Curve to project them onto the surface of said part.

Anyways, I ran into another problem. I'm trying to use the Extrude tool to subtract the shape of the symbol into the surface of my part.
It's a pre-made symbol, composed of 61 splines/curves. But whenever I try it, I get the error in the image below:

"Alerts: Unable to create body - change the section."

What am I doing wrong?

 

[cowski]

Do any of the curves in the symbol intersect (either themselves or each other)? Are there any other issues with the curves that would result in a non-manifold solid in the extrude command? Is the surface that you projected the curves to planar? The extrude command works best with a planar section of curves; it has a limited ability to work with non-planar sections, but you are more likely to run into problems.

www.nxjournaling.com

 

[JohnRBaker]

Also your 'End Distance' is LESS than the modeling tolerance. Try changing the modeling tolerance by an order of magnitude to 0.00254.

BTW, just as a heads-up, starting with NX 10.0, the default, out-of-the-box, modeling 'Distance' tolerance has been changed to 0.0100 mm and 0.0004 inches (the default 'Angle' tolerance has not changed).

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[who8myrice123]

Hey guys, thanks for the help!
John, changing the tolerance and end distance fixed the problem, thank you!
Also, one more question: is it ideal to simply change the tolerance for a problem such as this? I feel like its a simple shortcut around the problem.
Nonetheless, thanks guys!

 

[JohnRBaker]

Actually if your typical models are small, say less than 2 meters (78 inches) in size, I would change your overall default modeling tolerance to the new 'standard', that is 0.0100 mm (0.0004 inches).

BTW, the reason for our recent change in the default modeling Distance tolerance is because over the years, the size of tha typical piece part modeled by our customers using NX has become smaller. When Unigraphics was first developed back in the mid- to late-70's, many of our customers were in the aerospace sector (after all, for years Unigraphics was developed and sold by McDonnell Douglas). However, over the last 20 years or so, our 'sweet spot' in the industry has moved toward automotive, where the typical piece part size is much smaller. Therefore, starting with NX 10.0 we've switched our default Distance tolerance to the standard that was adopted by the majority of the automotive OEM's and their suppliers, that is 0.0100 mm (0.0004 inches). But as always, these default tolerances can be changed and they should be reviewed when purchasing CAD and selecting something appropriate for your particular product line.

As for your question about is it OK to set the tolerance for a single operation, the answer is YES. After all, why do you think we include an option to set the tolerance inside of specific modeling functions. But note that changing the tolerance values while in a feature dialog will ONLY effect the tolerance used for that particular operation and will have no impact on the default (AKA pre-set) modeling tolerance that was saved with the part file. However, changing the tolerance in Preferences -> Modeling and saving the part will change it for any subsequent modeling operations but it will have no impact on features already created. Also note that not all modeling operations are affected by the tolerance settings. Generally speaking, those features or operations where tolerance is a factor, those are the ones where you'll find a tolerance option in the settings section of the dialog. Also note that for most of these features, the tolerance itself will be become part of the parametric values of that particular feature, often even showing-up as its own expression. And before you ask, there is no way, at least not as part of an interactive operation, to change the tolerance of all of the features of a model. Please note that while there are some CAD systems which does allow you to do that, Pro-E comes to mind, it is generally NOT something that you should be doing as it can be problematic and so we decided years ago to not provide a way to do that. If you feel that you need to tighten or loosen the tolerance on your models, for whatever reason, it should be done on a feature by feature basis so as to know exactly how this will impact the results and the reliability of updating.

Anyway, I thought that you should know how all this works and why.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[UG39]

Hi JohnRBaker ;
Just wondering why when I change Tolerance for modeling (general- distance) in customer default from .0004" to .001" (NX10) in default level (user)
after restarting NX , still G0 position in modeling (surface creation i.e. sweep , mesh,... ) remain unchanged to default .0004

 

[cowski]

Changing the customer defaults only affects new (blank) files. To change the modeling tolerance in an existing file, open the file and go to Preferences -> modeling -> general and change the distance and angular tolerance values.

www.nxjournaling.com

 

[JohnRBaker]

cowski is correct, but I have to ask, why are you changing your Modeling Tolerance? Now there's no problem changing it (after all if we didn't want you to change it, we wouldn't have given you the option) it's just that we would like to know what your motivation is. Call it professional curiosity if for no other reason ;-)

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Toost]

In this particular case, you have a "symbol" of imported splines.
Despite the NURBS standard, there are a couple of things that can be done to splines within the Nurbs standard which NX doesn't like that much. Have a look at these curves and see if you can re-create or clean them in NX in a simple way.
having clean curves will produce clean faces which updates quickly and produce small files which opens quickly...

Regards,
Tomas

 

[UG39]

John;
I knew about opening new model to take in effect but,
Actually I tested it does not change even with new model creation?! in my case
when I check in customer default tolerance is correct as I defined .001" but
in functions still it shows .0004"
attached shows after changing tol. to .001"
thanks

 

[cowski]

Did you create a new file by using the "Blank" template? Using the blank template will create a brand new file based on the customer defaults. Any other template option (model, assembly, sheet metal, etc) will base the new file on an existing file (essentially performing a "save-as" on an existing file, a "template", that you or someone else created). If you want the change to apply to these template files, you will need to open the template file, change the tolerances in the modeling preferences, and save the file. Now new files based on the template will use the same settings as the template.

www.nxjournaling.com

 

[UG39]

cowski;

Thank you that is the point creating in blank template update whatever Tol. defined
Problem Solved
Thanks again

 

[JohnRBaker]

I'm still interested in what is motivating you to use a different default Modeling Tolerance.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Digital Factory
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.